Siemens SINUMERIK 840D sl Operation/Programming Manual page 224

ShopTurn Functions
5
5.4 Contour turning
Rounding at the contour
Cut segmentation
Set machining area
limits
Feed interruption
Machining type
5-224
In order to avoid residual corners during roughing, you can enable the
"Always round the contour" function. This will remove the protrusions
that are always left at the end with each cut (due to the cut geometry).
The "Do not round contour" setting accelerates machining of the
contour. However, any resulting residual corners will not be
recognized or machined. Thus, it is imperative that you check the
behavior before machining using the simulation.
When set to "automatic", rounding is always performed if the angle
between the cutting edge and the contour exceeds a certain value.
The angle is set in a machine data code.
Please also refer to the machine manufacturer's instructions.
To avoid the occurrence of very thin cuts in cut segmentation due to
contour edges, you can align the cut segmentation to the contour
edges. During machining the contour is then divided by the edges into
individual sections and cut segmentation is performed separately for
each section.
If, for example, you want to machine a certain area of the contour with
a different tool, you can set machining area limits so that machining
only takes place in the area of the contour you have selected.
You can define between 1 and 4 limit lines.
To prevent the occurrence of excessively long chips during machining,
you can program a feed interruption. Parameter DI specifies the
distance after which the feed interruption should occur.
The interruption time or retraction distance is defined in machine data.
Please also refer to the machine manufacturer's instructions.
You can select the machining mode (roughing or finishing). During
contour roughing, parallel cuts of maximum infeed depth are created.
Roughing is performed up to the final machining allowance
programmed.
You can also specify a compensation allowance U1 for finishing
operations, which allows you to either finish several times (positive
allowance) or to shrink the contour (negative allowance).
Finishing is performed in the same direction as roughing.
SINUMERIK 840D sl Operation/Programming ShopTurn (BAT) – 08/2005 Edition
08/2005
5
♥ Siemens AG, 2005. All rights reserved